
[Sponsors] 
Mesh Refinement vs Residual/Convergence in Turbulence 

LinkBack  Thread Tools  Search this Thread  Display Modes 
February 22, 2019, 09:57 
Mesh Refinement vs Residual/Convergence in Turbulence

#1 
New Member
Joshua Brickel
Join Date: Nov 2013
Posts: 25
Rep Power: 8 
I was hoping someone can help me get insight into the issue of meshrefinement vs. convergence issues.
Firstly my setup: I have a cylinder inside a cylinder. The outer tube has two openings 180° apart from each other. The flow enters and leaves through these holes. The flow is thus forced to go around the inner cylinder. But due to the outer cylinder the flow is fairly confined and there is a quite a bit of wall effect. I am in the turbulent regime, and hence due to the large amount of wall effect I chose the SST turbulent model. I am running this as a RANS Steady State. I ran the solution at various flow rates. Convergence was good. But I wasn't sure if the solution was accurate, that is if my solution was mesh independent. So I decided to refine the mesh. I basically created a mesh with 4x the number of elements. At high velocity flows the convergence is a lot worse. But the value of interest (pressure loss across the flow path) also changed quite a bit (about 15 to 20% different). And before anyone asks, I tried running with double precision, but no change was observed in the residual levels. The high residuals occur on the far side of the inner cylinder where the flow around the cylinder converges back together. My working assumption is that I have refined too far and I am now picking up some of the larger scale eddies. But now I am stuck with a conundrum. 1) The change in mesh size seems to indicate that the mesh wasn't refined enough for high flow rates (in that the value of interest significantly changed). 2) The change in mesh size seems to be have picked up some of the larger scale eddies, preventing the residuals from going to a decent level for convergence. So is the only way I can now tell at high flow rates if my mesh resolution was sufficient would be for me to run the solution as transient? Any insights would be appreciated. 

February 22, 2019, 11:31 

#2 
Senior Member
Join Date: Jun 2009
Posts: 1,111
Rep Power: 22 
What happens if you change the timestep?
Say increase it (which can make it unstable or converge bette), or decrease it (which may relax it a bit more) 

February 22, 2019, 11:48 

#3  
New Member
Joshua Brickel
Join Date: Nov 2013
Posts: 25
Rep Power: 8 
Quote:
However when thinking about it, wouldn't increasing the pseudo time step work against the reason I made a finer mesh. My logic is that isn't the code now so to speak numerically diffusing the results from one cell over additional cells. As for lowering the time step. That may lower the standard residuals, but I would think for the pressure differential I am looking for it would just simply slow down the peaks and valleys I see in the steady state solution, but not alter them. If you feel I am misinformed about one or both of these issues, I would be happy to hear your logic. Last edited by JoshuaB; February 22, 2019 at 12:10. Reason: clarity 

February 22, 2019, 12:45 

#4 
Senior Member
Join Date: Jun 2009
Posts: 1,111
Rep Power: 22 
For steadystate cases, the value of the timestep has absolutely no influence on the results if the simulation is converged. Any dependence on the timestep is a defect and a bogus solution.
However, the timestep size has a very strong influence on how fast/slow the solution converges, or if it converges at all. Summary: timestep value is your knob to guide convergence, and it sure is related to some physics, but the final results do not depend on it. 

February 22, 2019, 14:28 

#5 
New Member
Joshua Brickel
Join Date: Nov 2013
Posts: 25
Rep Power: 8 
Thanks. So I guess in order to see if a steady state solution exists I need to try both increasing and decreasing the time step.
I think I understand the the decreasing the time step. My thought is that decreasing the pseudotime step to try is analogous in Pressure based solvers of lowering the relaxation factors. So I see how this makes sense. If their is a converged steady state solution this is one way to ferret it out. However I'm a bit more confused why increasing the pseudo timestep should work just as well. I can see how it would make things less stable, once again, similar to the making the relaxation factors too large. I'm just not sure how it can make the solution converge better. If you can help me with a justification for this I would appreciate it. But at any rate, if these methods don't increase the solutions ability to converge, then I take it the solution is probably inherently unsteady. 

February 22, 2019, 17:04 

#6 
Senior Member
Join Date: Jun 2009
Posts: 1,111
Rep Power: 22 
Recall the use of a "false timestep" approach is trying to approximate a transient solution (all the physics in sync among all equations).
A very small timestep would approach a transient solution; however, ANSYS CFX also introduces other relaxation factors which prevent it from being a true transient. As you decrease the timestep size, the iterative process may capture some features (similar to a true transient), and those features can prevent convergence or increase the number of iterations to steady state convergence. As you increase the timestep, you may overcome those; however, at the risk of making it unstable. That is, there may be "sweet spot" . 

February 23, 2019, 04:37 

#7  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,980
Rep Power: 122 
My 2c worth:
Quote:
Increasing the pseudo time step size in a steady state simulation which is not converging well is trying stabilise the small flow features which are likely moving around (ie transient). If the pseudo time step is too large to resolve these flow features then they are smoothed out and a steady state flow field is achieved. Well, that is the theory anyway. It does not always work but is definitely worth a try. But your comment that your mesh refinement requires a transient simulation for convergence is correct. If you cannot obtain convergence by adjusting the pseudo time step size as Opaque suggests then you have to do it transient. But before you do, don't forget that the convergence criteria is also a parameter you should do a sensitivity study on. If you find you don't need to converge as tightly as you currently do then you might avoid this whole problem of convergence on fine meshes as a looser convergence could be OK.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

February 25, 2019, 09:31 

#8 
New Member
Joshua Brickel
Join Date: Nov 2013
Posts: 25
Rep Power: 8 
So if I understand you and "Opaque" correctly, refining the mesh and increasing the time pseudotimestep will not work against each other. That is the mesh will solve with the accuracy of a refined mesh. Just some of the small scale affects which are transient in nature (and unimportant in the steady state solution) are being numerically diffused out.
The reason I created this refined mesh was to see if I was truly mesh converged (which I was not at the larger mesh). So this purpose will not be affected by increasing the psuedotime step. However if even in increasing and decreasing the time step my residuals, and more importantly, my variables of interest continue to bounce around at too high a level, then at that point I do need to perform a transient solution. Would you say this is an accurate understanding? 

February 25, 2019, 20:16 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,980
Rep Power: 122 
Yes, that sounds correct.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Tags 
convergence, mesh refinement study, turbulence 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[snappyHexMesh] problems generating clean mesh  Christian_tt  OpenFOAM Meshing & Mesh Conversion  2  June 20, 2019 06:39 
decomposePar problem: Cell 0contains face labels out of range  vaina74  OpenFOAM PreProcessing  32  February 7, 2018 09:26 
[snappyHexMesh] Creating very fine, high accuracy mesh with snappyHexMesh  JD_Welch  OpenFOAM Meshing & Mesh Conversion  9  November 17, 2017 01:46 
[snappyHexMesh] Removing further cells after SHM  zonda  OpenFOAM Meshing & Mesh Conversion  14  September 15, 2017 08:50 
[snappyHexMesh] SnappyHexMesh running killed!  Mark JIN  OpenFOAM Meshing & Mesh Conversion  2  October 4, 2016 01:19 